Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Tool center vs Tool Tip

Message 1 of 2
157 Views, 1 Reply

Tool center vs Tool Tip

I have been working on a 5th Axis machine. It does have TCP option but it's a relatively cheaper machine that cannot properly complete the calculations to switch the toolpath data to compensate for the tool diameter. 

For example, Mastercam has an option to do calculation from the tool tip(contact point) or from the center of the tool.

Does this option exist or some way to implement it within the Post processor? We tried cutting a 5th axis part and ended up with the tool floating about 6mm (using a 12mm Diameter Ball End Mill) from the expected toolpath. Another that was one of Fusion's truly 5th axis toolpaths wasn't cut to the proper depth, appromixately 6mm all around was left on the part.


Like the picture I have attached for better understanding.



Message 2 of 2

In MasterCAM some of the toolpaths call this Tip Comp.  This is where you tell the CAM software how to calculate the toolpath.  If you touch-off your tools at the Tip, then use Tip in the CAM software.  If you use the center of the tool radius as the zero point for referencing your tool in the CNC machine, then you want the CAM software to calculate the toolpath using Center Compensation.  Either way is capable of generating the exact same toolpath.  


However, if you mix the two (Touch-off the tool at the TIP and set the CAM software to calculate the toolpath at the CENTER) you will have problems.  I'm guessing you touched off on the TIP of the tool (like most people do) but calculated the CAM toolpath in CENTER mode.  


In my experience, there are very few situations where you want to use CENTER mode.  All of the F360 3D and Multi-axis toolpaths would be in TIP mode and they expect you will touch the tool off on the tip (which is the most common way to do it).  I can't think of any benefit of using CENTER mode compared to TIP.  Perhaps someone else will chime in on that topic.  




I think you may be confusing 3D Cutter Compensation (G41.2 or G42.2) with Tilted Work Plane (G68.2) and Tool Center Point Control (G43.4)


3D Cutter compensation is complicated.  There are actually two different types - the more "simple" type comps the tool in a plane which is perpendicular to the axis of the tool and is would would be used with a SWARF toolpath.  The more complex type of 3D cutter compensation gives the control a lot of data: The contact point (XYZ), the Surface Normal (UVW) and the Tool Vector (IJK).  Not every CNC control is capable of doing this advanced type.  Most CNC machinists work their entire career and never use this feature.  


Tilted Work Plane (TWP) is much more common and you will see it in most every 3 + 2 program.  You will also see it in 5-axis programs along with G43.4 TCP.

Now, if you are saying your CNC control can't do TWP (G68.2) or TCP (G43.4) then you have a different problem.  You will have to place your program WCS at the physical intersection of the rotary axes.  If you feel you need Tool CENTER mode in this scenario, then you won't be using F360 as all of the toolpaths calculate in Tool TIP mode.  That said, I've seen many non TWP/TCP machines running multi-axis program with toolpaths calculated in Tool TIP mode.  It's not convenient, but it does work.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report